Solidworks Import Limitations
Ray,
I'm sorry to hear you are still having problems with the workflow. Let's try to get on the same page here.
This is what I'm doing to upload and edit the file you provided:
If these steps don't work for you, I need more information to try and reproduce your problem.
1. What is your OS?
2. Can you make a video using Autodesk Screencast (it's free), and show us the steps you are taking?
Thanks,
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Noted. We're already looking at this model regarding that failure/related failures. So the pocket will get looked at.
In the mean time, you aren't limited by Find Features. There are other direct editing tools such as Press Pull and Move (with face option).
Here is Press-Pull in action on the pocket.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
I know a number of 3D CADpackages, CATIA, Solid Works, Solid Edge, Geomagic Design. To my knowledge no commercially available CAD package can import files from another CAD While retaining the full design history.
Fusion 360 certainly does not. The timeline is unique to Fusion 360 and feature trees from
Other CAD packages are not 1:1 mappable to the timeline.
Fusion 360 certainly does not. The timeline is unique to Fusion 360 and feature trees from
Other CAD packages are not 1:1 mappable to the timeline.
Thanks for your help on this.
Same to you. 🙂
@Anonymous
To be clear, we can totally reproduce this and are working to improve Fusion based on your report and model file. Thanks for posting!
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
@Anonymous
Regarding your PS:
Can you open a new thread on this forum and provide examples of where noun > verb input fails in Fusion? Just list all the commands that don't work when you select something and then try to use the command you want. Sounds like a great discussion!
Regards,
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Hi guys
In my previous post I've said I will make a screencast, and I was trying yesterday... but I just couldn't conclude, after 30 minutes I wasn't even in the middle.
Who would watch that? That why I've decided to write this post. I should be at least able to make an ordered statements.
There are three things I would like to speak about. First, I want to explain what Find Feature means indeed. Mainly because I suspect that's the main problem that Ray has.
Secondly, along this thread we have came across at least two bugs, and I think I can point what's causing them.
Et the end I would like to show, how we can utilise "dummy" geometry in parametric environment.
It's gonna be a simple example, where I intentionaly define prismatic part in Direct Modeling environment, to build on that a paramertic model.
1. Find Feature is not abuot recreating features that were used to create certain geomerty.
To understand that, we need to know what's the different between features that we can see in parametric mode and the features in direct mode.
Icons looks the same, geometries created by those feature are the same in both modes.
In parametric modeling available tools create geometry (bodies, surfaces) and features. Those features store all inputs that were used for geometry creation.
When we editing feature, we re-enabling tool with all inputs.
In direct mode, tools also create geometries and features, but this time features don't store initial inputs. What features store are "definitions" of created geometry.
I've used brackets, because it's not an exact term, rather illustrative description. Then how to understand that therm?
I will need two examples, one will be loft feature/tool and a second one, chamfer.
On image above I've created transition between two boxes with a loft tool. Data used to create that transition are two faces as profiles and eight faces to match tangency.
In parametric mode those data would be preserved for futher use, in direct mode we don't have data preseved, and all data we need to extract from geometry itself.
Problem is that, our body after loft don't have faces which we used as profiles. We can argue, that we have edges of those faces, so it should be possible.
If so then look at this illustration:
I've removed some of our body, and now geometry have even less data to try recreate loft feature.
With that type of tools, we still gonna see loft feature in browser, but without option to edit them.
Second example is a chamfer.
On image below I've draw rectangle with cut down corner, and I've extruded that sketch in to a solid body. Initialy our solid is solved/"defined" as single extrusion.
Nevertheless, same body we could get by numerous other operation. For example I could add a chamfer to an edge of a box.
What kind of data we need to fully define chamfer?
Adjacent faces, chamfer widht and angles. All those data we have within our model. To make it visually obviouse I've painted faces I'm talking about.
In direct mode features like chamfer are editable, because we have all geometry that defines that feature.
Finally I get to the point. Find Feature tool is capable of finding geometry interdependency. Those dependencies could match certain feature.
Equally distant holes, could be part of rectangular pattern, or circular pattern. Which one is correct is determed by purpose.
Because algorith can't guess that, based on geometry it self, we have a dialog window, where we can specify which dependency Fusion should look for.
Find Feature is very useful, but because it uses term "feautre", we could make wrong assumption based on features in parametic mode.
In your case it may look useless. But even if, you still can build parametric model, having non-parametric "inserts". You just need to treat Find Feature differently.
Majority of warnings we see, beacuse given data are not enough to solve certain features (definition is not complete).
On first try, Find Feature can solve part in a way you wouldn't expect. Then you need to unsolve those features (Dissolve), and specify what you need (yes only from availble option).
If it still struggle, you can even pick only those faces that are needed for feature to be solved.
What's important, is that one set of faces could be one feature only, it can't be solved as two different features.
2.Now it's time to talk about bugs.
If anyone get to this point, should understand immediately, that for people unfamiliar with direct modeling, bugs we came across could only make it more confusing.
First bug Ray was pointing, was that he couldn't edit any feature on a solved part (of course Ray in his first post, was saying also about other problems, but non of them was a bug, indeed).
I've looked on his model, and first thing I've noticed, was that I'm in parametric mode.
Where if that would be a simple edit of solidworks file, I should start in direct modeling environment.
First thing I've done to trace the bug, was to check original .sldprt file. Maybe bug occures with first Find Feature use, after initial translation?
But everything was ok (almost, second bug have appeared), I was able to edit features.
Clue was trivial, something was happening when we moved from direct modeling in to parametric modeling.
There are two ways we can make that move. First, start capturing history on imported file. That creates Base Feature in a timeline.
Base Feature is editable, and this way we get access to our part. Unfortunately, this way features were still editable, no errors.
Second way to get our part (DM) in to parametric mode, is to insert that part in to another parametric file (Insert into Current Design).
That creates linked part. Only way to edit that insert, within same file, is to remove external association (Break Link).
After that I had access to features (through editing Base Feature), but our bug occured, and I wasn't able to edit any of regonized features.
That time I've write post, where I said that Break Link might be responsible for that bug. And I was wrong.
Because there was not much help just in tracking bug. I've tried to find workaround.
Simplest idea was to copy body form original file to fresh one (baisicly copy instead of Insert into Current Design).
In order to do that first thing we need is to manualy create Base Feature, and then "inside" that Base Feature paste the body.
Workaround works perfectly, features are editable. That's a good news but, when I've looked at Ray file again, there was one more detail different.
In his timeline before Base Feature we have one more feature, New Component.
Obviesly it's there after breaking a link, but what gonna happen if I'll try to mimic that file structure and use my "copy/paste" trick?
I've created new component (by defaulf it was automaticly activated), then created Base Feature, and eventualy paste body.
Our bug appeared again? That give me a clue that bug's appearing when part is copied in to component on a lower level (in to subassembly).
To prove me being right, I had to create new component, but this time after that, I had to activate top level component.
When I've created Base Feature it was refering to top level, and pasted body landed on that level also. Quick check, and everything was ok.
Conclusion is simple, copied body need to be pasted to top level component, in a same time it's the only rule we need to keep to workaround that bug.
Second bug we have seen, was when on originaly translated .sldprt file, we was unable to edit hole1, the one which Ray called pocked.
Way that Ray called that feature give me a clue. When I was trying to edit that hole, arrow manipulator was pointing opposite direction to cut that was performed.
All other holes also showed same direction when edited, but bacause they were through holes it was irrelevant for which plane they were cut from.
In a case of pocket it's irrelevant only if we use extrude tool/feature, because we can specify second direction (like offset in Solidworks).
In our case feature that was recognized on that geometry was a hole feature, which can't be defined from opposite side.
Clearly Find Feature assigned wrong plane to that specific feature. I don't know way, but I've noticed one more thing that might help developers to track that bug.
Take a look, what's happening on mirrored part:
I wish that someone get so far, and my effort wasn't pointless.
Last thing I'd like to do is, to convince Ray that using direct modeling might be useful for creating parametric models.
Some time ago, I was working on a model with very simple, even trivial geometry.
It was "totem" like, romboid prism. It has served as display stand, with touch screen. While geometry was simple it was tricky to make it parametric.
I knew only height (it was locked, for any reasons, on 1000mm), I also knew that it should lean toward user, and top surface with display should be tilted.
I didn't know how far it should lean, nor the angle for a display... even didn't konw the exact size of screen, that would be used.
So, everything except height should be adjustable. It was a riddle for me.
No matter how I define sketch, no matter what feature order I've tried, always at least one "parameter" was laborious to re-edit.
Of course whole concept of parametric model is about ability to re-edit features without destroying downstream features.
After some time, I've decide to start in direct modeling, to have freedom in shaping base body.
Here's a screencast:
Thsi is really an outstaning explanation of what Find Feature does.
I don't ususally work in direct editing, so with this explanation in mind I'l' certainly approach it more educated if I try DM.
I’ve been trying to upload a new assembly to Fusion 360. It doesn’t show any signs of making progress. I uploaded it the same way that I uploaded a previous assembly (uploading all files in the assembly and choosing the top assembly file), but it just doesn’t seem to be working this time. Can anyone help me with this? I am currently uploading the assembly to mediafire so that I can share that link with someone that might be able to help me upload it to Fusion 360. This is all that I see. I left it uploading overnight. No progress.
It's possible the translation service is confused about the assembly structure. Do any of the sub assemblies contain sub assemblies?
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.